Re: gEDA-user: gEDA code sprint this coming weekend (April 3rd)

[DJ Delorie <dj@xxxxxxxxxxx>]

> DJ I've not tried the new importer but if you'd provide a pointer to
> instructions, I'll be glad to give it a try on the 4 boards I have
> in development now.

In general, the importer is best used for the "simple" case (although
it supports more complex cases):

If you have some schematic foo.sch

and you want a board foo.pcb

Create a blank board in pcb and save it as "foo.pcb"

Click File->Import schematics



For more complex boards, you need the Import() action's instructions
(note that there's an Edit->Board Attributes for setting the
attributes noted below):


static const char import_syntax[] =
  "Import()\n"
  "Import([gnetlist|make[,source,source,...]])\n";

static const char import_help[] = "Import schematics";

/* %start-doc actions import

Imports element and netlist data from the schematics (or some other
source).  The first parameter, which is optional, is the mode.  If not
specified, the @code{import::mode} attribute in the PCB is used.
@code{gnetlist} means gnetlist is used to obtain the information from
the schematics.  @code{make} invokes @code{make}, assuming the user
has a @code{Makefile} in the current directory.  The @code{Makefile}
will be invoked with the following variables set:

@table @code

@item PCB
The name of the .pcb file

@item SRCLIST
A space-separated list of source files

@item OUT
The name of the file in which to put the command script, which may
contain any @pcb{} actions.  By default, this is a temporary file
selected by @pcb{}, but if you specify an @code{import::outfile}
attribute, that file name is used instead (and not automatically
deleted afterwards).

@end table

The target specified to be built is the first of these that apply:

@itemize @bullet

@item
The target specified by an @code{import::target} attribute.

@item
The output file specified by an @code{import::outfile} attribute.

@item
If nothing else is specified, the target is @code{pcb_import}.

@end itemize

If you specify an @code{import::makefile} attribute, then "-f <that
file>" will be added to the command line.

If you specify the mode, you may also specify the source files
(schematics).  If you do not specify any, the list of schematics is
obtained by reading the @code{import::src@var{N}} attributes (like
@code{import::src0}, @code{import::src1}, etc).

For compatibility with future extensions to the import file format,
the generated file @emph{must not} start with the two characters
@code{#%}.

If a temporary file is needed the @code{TMPDIR} environment variable
is used to select its location.

Note that the programs @code{gnetlist} and @code{make} may be
overridden by the user via the @code{make-program} and @code{gnetlist}
@code{pcb} settings (i.e. in @code{~/.pcb/settings} or on the command
line).

%end-doc */


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user